I'm trying to determine peak stress in a lower wishbone insert. The part has a compound load case applied, one leg of the wishbone in tension, one in compression, and a load on the mount bracket in double shear through the pushrod, see below.

In practice, the only constraint is that the spherical joint cannot translate, but rotation is permitted in all axes. Initially, I applied an advanced fixture on the spherical face which mimics the internal surface of the bearing housing, and applied the condition that radial displacement must equal zero. With this applied, the insert appears to displace correctly given the applied forces, yet I get huge artificial stress concentrations around the inside circumference of the spherical surface, see below.

The above result is achieved if I use an adaptive loop mesh. With a generic, fine mesh, the following is achieved.

I'm sure this isn't an uncommon thing to try and simulate, so hopefully there is a way to do this. In the meantime I am attempting to simulate the assembly, with the bearing included, using component contact fixtures and attempting the simulation by fix the bearings 'ball' instead.

This is the kind of thing that FEA is bad at--bolted joints, welds, rivets, bearings. Accurately simulating the force transfer between two components is really touchy, because a lot of the important effects depend on things that are difficult to know. You can do this type of analysis, but I wouldn't normally trust the results unless you take a pretty advanced approach.

I normally approach something like this by using FEA to design the bracket. Then I design the bearing attachment to the bracket using handbooks, hand calcs and manufacturers recommendations. Usually, straightforward F/A type bearing stress calculations are sufficient.

It's a shame because it's something you instinctively think should be quite simple for it to handle. The problem I'm facing is that I can't even design the bracket part using FEA because there seems to be no built-in constraint that will ensure the load is reacted in the correct way; if I just completely fix the inside of bearing bore, it will introduce load reactions that aren't there, and induce bending moments that aren't there.

If it was possible to constrain virtual geometry, such as a point in a sketch attached to the model, rather than only physical features, it would make things a lot easier.

It's a shame because it's something you instinctively think should be quite simple for it to handle. The problem I'm facing is that I can't even design the bracket part using FEA because there seems to be no built-in constraint that will ensure the load is reacted in the correct way; if I just completely fix the inside of bearing bore, it will introduce load reactions that aren't there, and induce bending moments that aren't there.

If it was possible to constrain virtual geometry, such as a point in a sketch attached to the model, rather than only physical features, it would make things a lot easier.

You can using a remote displacement; you'll need to create a Coordinate System at the center where you want the rotations to act about, and then define the translations to be 0 and the rotations to be free.

You mention you were also trying to simulate the assembly by restraining the bearing's translation rather than the bore's translation. That seems a reasonable approach to me since it should move the stress concentration away from the bore, unless the contacts cause a problem. I'd be interested to hear how that goes.

Do you mean add the outer race of the bearing rather than change the insert to mimic the geometry of the outer race?

If so, I just wanted to isolate the two possible difficulties, so primarily try to get the spherical constraints working correctly, without having to worry about whether the component contact is working correctly too. I appreciate this may seem unintuitive, but it's been a few years since I did any FEA, especially with Solidworks.

If you mean adding in the bearing and performing the study on the entire assembly, this is what I'm attempting now, with difficulty, since it returns an error that there are insufficient fixtures. I'm trying now to work out exactly where this problem arises.

If you mean adding in the bearing and performing the study on the entire assembly, this is what I'm attempting now, with difficulty, since it returns an error that there are insufficient fixtures. I'm trying now to work out exactly where this problem arises.

This error is most likely due to one of the components that you added in going through rigid body motion. Make sure you have enough constraints such that you model can freely translate or rotate; also keep in mind that balanced loads do not prevent rigid body motion. If the correct nature of the model requires balanced loads to "prevent" rigid body motion, then add in a few soft springs to stabilize the model.

see shaun's response regarding replacing the components with a restraint

but yes, my suggestion is to add the next component and contact between it and the component you are trying to analyze. it adds complexity but removes the need to virtualize the restraint/contact. you're at a simple enough level from an assembly perspective, this is still a worthy direction.

As Mike pointed out, connections get very tricky to handle properly with FEA, particularly when you restrict yourself to a linear assumption for a connection that works on contact. That being said, there are ways mimic the nature of the connection (as Mike mentioned) that have different levels of refinement.

The key characteristics of a ball joint that you want to capture are:

It's stiffness.

The load transfer via the contact patch.

The first item is the easiest to do and there are twos ways I can think of doing it in SW are:

A remote displacement between the inner surface and a point at the center of the hole. For this, you'd have all translations at the point set to 0 and all rotations set as free (i.e. an unknown).

A short beam element where on end of the beam is fixed and the only end of the beam is linked to the inner surface of the hole. With this, you defined beam releases such that all translations at that end of the beam were locked but all rotations were free.

The first item is going to act just like a constraint, while the second will introduce a little flexibility (depending on the length of the beam, its cross-sectional properties, and material properties). However, both ways result in the inner surface being infinitely rigid due to the connection method SW uses, and I'm not sure if SW provides a different method (maybe others mode fimilar with the software will know whether SW allows the uses to change from a rigid link (e.g. RBE2 in Nastran) to a weighted link (e.g. RBE3 in Nastran)).

Mimicking the contact pad can be done by dividing up the inner surface of the hole such that you have a sub-region that is roughly the size and location of the contact pad and then applying your connection method over that sub-region. The size and location of the sub-region is based on engineering judgement (initially), and can be refined by looking a vector plot of the maximum and minimum principle stresses to minimize areas that have tensile stresses (a contact connection only carries compression and some shear from friction).

As you can imagine, this can be somewhat tedious and how smoothly it goes depends on the skills of the analyst. Even then, this is at best an approximation of the nature of the joint. Depending on the specifics of the model and the goals of the analysis, it could be easier (and even faster) to setup a contact problem.

Thanks all for your input on this, really appreciate it and it's helped me get to a point where I can consider my results to be representative, much more that I had previously!

I was able to apply the remote constraint to a coord system at the centre of the ball joint succesfully. This appears to react the loads I apply and allow movement correctly. I did attempt to model this is an assembly and use component contacts, to no avail. I was underconstraining the model somewhere regarding the connections. It's not something I've tried before so I will be attempting to understand this at a later date, to hopefully give a more realistic view of load transfer at the copponent interfaces.

Thanks again for your time, I will try to update if I can get the latter method to work.